To configure settings on the Basic tabbed page:

In the Edit Step dialog box, display the Basic tabbed page.

(For information on displaying the Edit Step dialog box, see “Creating a step,” Section 14.9.2, or “Editing a step,” Section 14.9.3.)

In the Description field, enter a short description of what occurs during this analysis step. ABAQUS stores the text that you enter in the output database, and the text is displayed in the state block by the Visualization module.

From the list of Eigensolver options, select Lanczos.

Select one of the Number of eigenvalues requested options to indicate how many eigenvalues you want calculated:

Select All in frequency range if you want ABAQUS/Standard to calculate all the eigenvalues within a range determined by a maximum frequency value (and, if desired, a minimum frequency value) that you enter.

Select Value if you want a particular number of eigenvalues to be calculated. Then enter that value in the field provided.

Toggle on Frequency shift (cycles/time)**2 to specify a positive or negative shifted squared frequency, S. If you toggle this option on, enter a value for the frequency shift in the field provided. For more information, see “Frequency shift” in “Natural frequency extraction,” Section 6.3.5 of the ABAQUS Analysis User's Manual.

Toggle on Minimum frequency of interest (cycles/time) to specify a lower limit to the frequency range within which ABAQUS/Standard will calculate eigenvalues. If you toggle on this option, enter a value for the minimum frequency in the field provided.

This option is required if you intend to use the Lanczos solver in parallel mode.

Toggle on Maximum frequency of interest (cycles/time) to specify an upper limit to the frequency range within which ABAQUS/Standard will calculate eigenvalues. If you toggle on this option, enter a value for the maximum frequency in the field provided.

This option is required if you intend to use the Lanczos solver in parallel mode.

If the model includes acoustic and structural elements coupled together or ASI-type elements, you can toggle on Include acoustic-structural coupling where applicable to include the effect of acoustic-structural coupling during the frequency extraction. (This option is toggled on by default.) For more information, see “Acoustic-structural coupling” in “Natural frequency extraction,” Section 6.3.5 of the ABAQUS Analysis User's Manual.

Specify your preference for block size:

Select Default to use the default block size of 7, which is usually appropriate.

Select Value to enter a particular block size. Then enter that value in the field provided. In general, the block size for the Lanczos method should be as large as the largest expected multiplicity of eigenvalues.

For more information, see “Lanczos eigensolver” in “Natural frequency extraction,” Section 6.3.5 of the ABAQUS Analysis User's Manual.

Specify your preference for the Maximum number of block Lanczos steps:

Select Default to allow ABAQUS/Standard to determine the number of block Lanczos steps within each Lanczos run. The default value is usually appropriate.

Select Value to enter a limit to the number of Lanczos steps within each Lanczos run. Then enter that value in the field provided. In general, if a particular type of eigenproblem converges slowly, providing more block Lanczos steps will reduce the analysis cost. On the other hand, if you know that a particular type of problem converges quickly, providing fewer block Lanczos steps will reduce the amount of in-core memory used.

Toggle on Include residual modes to request that ABAQUS/Standard compute residual modes based on the loads specified in the immediately preceding static, linear perturbation step. For more information, see “Obtaining residual modes for use in mode-based procedures” in “Natural frequency extraction,” Section 6.3.5 of the ABAQUS Analysis User's Manual.

To configure settings on the Parallel Lanczos tabbed page:

In the Edit Step dialog box, display the Parallel Lanczos tabbed page.

(For information on displaying the Edit Step dialog box, see “Creating a step,” Section 14.9.2, or “Editing a step,” Section 14.9.3.)

Note:  If you do not want to run the Lanczos solver in parallel mode, leave the default values on the Parallel Lanczos tabbed page unchanged, and skip this procedure. For more information, see “Performing the eigenvalue extraction in parallel with the Lanczos solver” in “Natural frequency extraction,” Section 6.3.5 of the ABAQUS Analysis User's Manual.

Select a method for defining the frequency domain intervals:

Select Specify number of frequency intervals to allow ABAQUS/Standard to divide the frequency domain into a particular number of intervals. Then enter the desired number of intervals in the field provided.

If you select this option, enter a value in the Distribute intervals with bias field:

• If you want ABAQUS/Standard to divide the frequency domain into equal size intervals, leave the default value of 1 unchanged.

• If you want the interval size to change gradually between lower and upper frequencies, enter an appropriate biasing parameter. For more information, see “Functionally biased splitting” in “Natural frequency extraction,” Section 6.3.5 of the ABAQUS Analysis User's Manual.

Select Specify interval boundaries to enter the frequencies that form the internal interval boundaries. Then enter those frequencies in the Interval Boundary column. The Minimum frequency of interest (cycles/time) that you specified on the Basic tabbed page will be the lower boundary to the first interval, and the Maximum frequency of interest (cycles/time) that you specified on the Basic tabbed page will be the upper boundary to the last interval.

To configure settings on the Other tabbed page:

In the Edit Step dialog box, display the Other tabbed page.

(For information on displaying the Edit Step dialog box, see “Creating a step,” Section 14.9.2, or “Editing a step,” Section 14.9.3.)

Accept the default Matrix storage setting. Since ABAQUS/Standard provides eigenvalue extraction only for symmetric matrices, steps with eigenfrequency extraction or eigenvalue buckling prediction procedures always use the symmetric matrix storage and solution scheme. You cannot change this setting. In such steps ABAQUS/Standard will symmetrize all contributions to the stiffness matrix.

Select an option for normalizing eigenvectors:

Select Displacement to normalize the eigenvectors so that the largest displacement, rotation, or acoustic pressure entry in each vector is unity.

Select Mass to normalize the eigenvectors with respect to the structure's mass matrix (the eigenvectors are scaled so that the generalized mass for each vector is unity).

For more information, see “Normalization” in “Natural frequency extraction,” Section 6.3.5 of the ABAQUS Analysis User's Manual.

Toggle on Evaluate dependent properties at frequency to evaluate frequency-dependent properties for viscoelasticity, springs, and dashpots during the eigenvalue extraction. If you toggle this option on, enter the desired evaluation frequency in the field provided. For more information, see “Evaluating frequency-dependent material properties” in “Natural frequency extraction,” Section 6.3.5 of the ABAQUS Analysis User's Manual.

To configure settings on the Basic tabbed page:

In the Edit Step dialog box, display the Basic tabbed page.

(For information on displaying the Edit Step dialog box, see “Creating a step,” Section 14.9.2, or “Editing a step,” Section 14.9.3.)

In the Description field, enter a short description of what occurs during this analysis step. ABAQUS/Standard stores the text that you enter in the output database, and the text is displayed in the state block by the Visualization module.

From the list of Eigensolver options, select AMS.

Toggle on Minimum frequency of interest (cycles/time) to specify a lower limit to the frequency range within which ABAQUS/Standard will calculate eigenvalues. If you toggle on this option, enter a value for the minimum frequency in the field provided.

In the Maximum frequency of interest (cycles/time) field, enter the upper limit to the frequency range within which ABAQUS/Standard will extract all the modes.

Toggle on Limit region of saved eigenvectors if you want to limit eigenvector computation to only the nodes in a particular region. If you toggle on this option, click the arrow to the right of the field provided to select the region of interest.

Toggle on Include residual modes to request that ABAQUS/Standard compute residual modes based on the static response of the model to a nominal (or unit) load.

If you toggle on this option, specify the residual mode regions and the degrees of freedom (DOF) for which you want residual modes calculated. ABAQUS/Standard computes one residual mode for every requested degree of freedom.

For more information, see “Obtaining residual modes for use in mode-based procedures” in “Natural frequency extraction,” Section 6.3.5 of the ABAQUS Analysis User's Manual.

To configure settings on the Other tabbed page:

In the Edit Step dialog box, display the Other tabbed page.

(For information on displaying the Edit Step dialog box, see “Creating a step,” Section 14.9.2, or “Editing a step,” Section 14.9.3.)

Accept the default Matrix storage setting. Since ABAQUS/Standard provides eigenvalue extraction only for symmetric matrices, steps with eigenfrequency extraction or eigenvalue buckling prediction procedures always use the symmetric matrix storage and solution scheme. You cannot change this setting. In such steps ABAQUS/Standard will symmetrize all contributions to the stiffness matrix.

In the Cut-off multiplier for substructure eigenproblems field, enter , the cut-off frequency for substructure eigenproblems, defined as a multiplier of the maximum frequency of interest. The default value is 5.

In the First cut-off multiplier for reduced eigenproblems field, enter , the first cut-off frequency for a reduced eigenproblem, defined as a multiplier of the maximum frequency of interest. The default value is 1.6. .

In the Second cut-off multiplier for reduced eigenproblems field, enter , the second cut-off frequency for a reduced eigenproblem, defined as a multiplier of the maximum frequency of interest. The default value is 1.3. .

For more information, see “Automatic multi-level substructuring (AMS) eigensolver” in “Natural frequency extraction,” Section 6.3.5 of the ABAQUS Analysis User's Manual.

To configure setting on the Basic tabbed page:

In the Edit Step dialog box, display the Basic tabbed page.

(For information on displaying the Edit Step dialog box, see “Creating a step,” Section 14.9.2, or “Editing a step,” Section 14.9.3.)

In the Description field, enter a short description of what occurs during this analysis step. ABAQUS/Standard stores the text that you enter in the output database, and the text is displayed in the state block by the Visualization module.

From the list of Eigensolver options, select Subspace.

In the Number of eigenvalues requested field, enter the number of eigenvalues that you want ABAQUS/Standard to calculate.

Toggle on Frequency shift (cycles/time)**2 to specify a positive or negative shifted squared frequency, S. If you toggle this option on, enter a value for the frequency shift in the field provided. For more information, see “Frequency shift” in “Natural frequency extraction,” Section 6.3.5 of the ABAQUS Analysis User's Manual.

Toggle on Maximum frequency of interest (cycles/time) to specify an upper limit to the frequency range within which ABAQUS/Standard will calculate eigenvalues. If you toggle on this option, enter a value for the maximum frequency in the field provided.

ABAQUS/Standard will extract eigenvalues until either the requested number of eigenvalues has been extracted or the last frequency extracted exceeds the maximum frequency of interest.

Enter a value for the number of Vectors used per iteration. In general, the convergence is more rapid with more vectors, but the memory requirement is also larger. Thus, if you know that a particular type of eigenproblem converges slowly, providing more vectors by using this option might reduce the analysis cost.

Enter a value for the Maximum number of iterations. The default is 30.

To configure settings on the Other tabbed page:

In the Edit Step dialog box, display the Other tabbed page.

(For information on displaying the Edit Step dialog box, see “Creating a step,” Section 14.9.2, or “Editing a step,” Section 14.9.3.)

Accept the default Matrix storage setting. Since ABAQUS/Standard provides eigenvalue extraction only for symmetric matrices, steps with eigenfrequency extraction or eigenvalue buckling prediction procedures always use the symmetric matrix storage and solution scheme. You cannot change this setting. In such steps ABAQUS/Standard will symmetrize all contributions to the stiffness matrix.

Select an option for normalizing eigenvectors:

Select Displacement to normalize the eigenvectors so that the largest displacement, rotation, or acoustic pressure entry in each vector is unity.

Select Mass to normalize the eigenvectors with respect to the structure's mass matrix (the eigenvectors are scaled so that the generalized mass for each vector is unity).

For more information, see “Normalization” in “Natural frequency extraction,” Section 6.3.5 of the ABAQUS Analysis User's Manual.

Toggle on Evaluate dependent properties at frequency to evaluate frequency-dependent properties for viscoelasticity, springs, and dashpots during the eigenvalue extraction. If you toggle on this option, enter the desired evaluation frequency in the field provided. For more information, see “Evaluating frequency-dependent material properties” in “Natural frequency extraction,” Section 6.3.5 of the ABAQUS Analysis User's Manual.